ABAQUS stent analysis failing
ABAQUS stent analysis failing
(OP)
I'm having some difficulty running a stent analysis and I'm hoping there might be some expertise here that can help me out. I just got done taking the online stent simulation tutorial from Simulia, and now I'm working to extrapolate on my own practice. I have a very simple laser-cut style 8- strut, single loope strut "stent" in 1/8 symmetry. It's nitinol, with an expand, recoil, and pressure steps. It fails about 0.73 through the expand step with time increments too small error. (general static step). I'm trying to define the nitinol with plasticity so I can overstrain it and model a good recoil behavior. My material model is as follows:
7232772.81
0.33
4403414.861
0.33
0.048987845
986.2584
65533.12968
68269.43497
0
986.2584
31662.44994
28827.94359
75637.317
0.0515
0
0
10
68312.898
0.065
90286.44508
0.06949
112303.6486
0.07449
156220.4298
0.08449
174045.6
0.09
184923.45
0.095
188549.4
0.1
190724.97
0.105
191450.16
0.11
192175.35
0.15
("units" are psi and C FWIW).
I've also tried eliminating the plasticity part and it still fails around the same time step. The max stress is only around 70 ksi, so it's still well within the material model. I've done "tricks" with nlgeom, and general solution controls I0, and Ir. I attached my cae file here.
Any thoughts why this won't converge?
7232772.81
0.33
4403414.861
0.33
0.048987845
986.2584
65533.12968
68269.43497
0
986.2584
31662.44994
28827.94359
75637.317
0.0515
0
0
10
68312.898
0.065
90286.44508
0.06949
112303.6486
0.07449
156220.4298
0.08449
174045.6
0.09
184923.45
0.095
188549.4
0.1
190724.97
0.105
191450.16
0.11
192175.35
0.15
("units" are psi and C FWIW).
I've also tried eliminating the plasticity part and it still fails around the same time step. The max stress is only around 70 ksi, so it's still well within the material model. I've done "tricks" with nlgeom, and general solution controls I0, and Ir. I attached my cae file here.
Any thoughts why this won't converge?





RE: ABAQUS stent analysis failing
Nitinol stents aren't expanded, Their initial shape is set through processing and heat treatment and they are allowed to expand freely in the target anatomy due to the shape memory property of nitinol.
Recoil only occurs with balloon-expandable devices when you deflate the balloon. There should be no recoil with a nitinol stent since there is no balloon.
There is an Abaqus/Standard benchmark analysis in the documentation that involves crimp and deployment of a nitinol stent. You can check that for guidance.
RE: ABAQUS stent analysis failing
I'll see if the documentation has something different than the test problem I was working on in the tutorial.
RE: ABAQUS stent analysis failing
If you're running into problems with shape set analyses, check the message file. Have force/displacement equilibrium been achieved? If not, you might have a problem with your boundary conditions. You can check the node and direction of the largest residual to see what portion of your model is causing problems and how it might not be constrained. What happens at 0.73 through the step? Do two parts come in contact? If so you might not have fully constrained one of them.
If contact hasn't converged you can adjust your interaction properties. Softened contact can help in these analyses. Where possible, avoid edge-surface interaction on your contact surfaces.
Also, if you think it's the material model, run it with linear elastic properties and see does it converge.
RE: ABAQUS stent analysis failing
Contact initiates almost immediately in the expand step. It quickly expands about 50% through the step, then bogs down. I ran the same model with the material model from ABAQUS, and it did complete, but with stress values an order of magnitude higher than what is possible. Just for completeness sake, here's the ABAQUS material model:
46728
0.33
25199
0.33
0.0426
4.5
358.2
437.8
0
4.5
124.25
17.75
537.3
0.0426
I'm hesitant to condemn my material model, because the two are so very close:
But on the other hand that one seemingly simple change really messes things up. Perhaps it's highlighting an issue somewhere else?
I'm running it right now with a linear elastic only "steel" model (no plastic definition at all), and I'll see if it completes.
RE: ABAQUS stent analysis failing
RE: ABAQUS stent analysis failing
RE: ABAQUS stent analysis failing
Have you tried rerunning the analysis with loosened contact constraints? What are you using for interaction properties at the moment?
RE: ABAQUS stent analysis failing
RE: ABAQUS stent analysis failing
Firstly, you're using inconsistent units. Your dimensions appear to be in meters but your stresses are in PSI. For consistency the stresses should be in Pa. Alternatively, scale your parts so they are in mm and adjust your stresses so they are in MPa - I find this much easier when modelling stents. Secondly, your transformation and volumetric transformation strains are different values. When this is the case, a different flow algorithm is used and the USYMM parameter is required on the *USER MATERIAL keyword. If you try to run the analysis without this parameter included you will run into convergence problems. Your model produced non-physical results with the Abaqus material model due to inconsistent units (dimensions are in meters but stresses are in MPa). Also, you did not have convergence problems with the Abaqus material model because the transformation and volumetric transformation strains are equal values.
When I addressed these problems your model ran fine. Here is the material model I used:
*Material, name=ABQ_SUPER_ELASTIC
*Depvar
24,
*User Material, constants=15, UNSYMM
4.9868e+10, 0.33, 3.036e+10, 0.33, 0.049, 6.80001e+06, 4.52e+08, 4.7e+08
0., 6.80001e+06, 2.18e+08, 1.99e+08, 5.22e+08, 0.0515, 0.
RE: ABAQUS stent analysis failing
Thanks also for the catch on the volumetric strain - you described exactly what I was running into. I'll go through and double check all my units, make the edit to the material model and try again. Thanks for bearing with me Dave!
RE: ABAQUS stent analysis failing
You should specify this and be aware of what properties are being used.